[RESOLU] flambement Sorensen si plusieurs _F de FORCE_POUTRE

J_Berthellemy

Bonjour,

Un problème semble bien apparaître quand on utilise la recherche des modes de flambement dans une structure à poutres par la méthode de Sorensen de MODE_ITER_SIMULT.

La prise en compte dans FORCE_POUTRE des cas de charges définis par plusieurs occurrence _F

est défectueuse et les résultats dépendent par exemple de l'ordre de définition des _F dans le .comm.

Résultats faux identiques dans la version 9 sous winfows et la version 10.02 sous linux.

Tous les _F ne semblent en fait pas pris en considération, mais aucun message d'erreur n'apparaît.

Cordialement.

jeanpierreaubry

bonjour

je retrouve ce post un peu par hasard

qu'enetdez vous par "plusieurs occurences de _F"

jean pierre aubry

J_Berthellemy

jeanpierreaubry wrote:
bonjour

je retrouve ce post un peu par hasard

qu'enetdez vous par "plusieurs occurences de _F"

jean pierre aubry

C'est très simple, avec le cas de charge suivant que je vous recopie :

Ch_ELU_R =AFFE_CHAR_MECA(MODELE=Structur,

FORCE_NODALE=(_F(NOEUD=('N33','N97','N161','N225','N289','N291','N227','N163', 'N99','N35',

'N34','N98','N162','N226','N290','N292','N228','N164','N100','N36',

FZ= -3.67*kelu/(2*102) ,), # poids metal des p_de_pont en MN = 3,67 tonnes /2

_F(NOEUD=('N13','N14','N15','N16',),

FZ= -kelu*(2*3.5 + 6.0)/(2*102) ,),), # poids des noeuds d'about et p_de_pont_about

FORCE_POUTRE=(

_F(GROUP_MA='GM1005', FZ= -(8.54/9.60)*4.19*0.25*2.6*kelu/102 ,), # poids de la dalle

_F(GROUP_MA='GM1001', FZ= -1.50*1.20*kelu/102 ,), # poids superstructures

_F(GROUP_MA='GM1001', FZ= -A_Tira*7.85*kelu/102 ,), # poids metal tirants

_F(GROUP_MA='GM1003', FZ= -A_Arcs*7.85*kelu/102 ,), # poids metal arcs

_F(GROUP_MA='GM1004', FZ= -A_Susp*7.85*kelu/102 ,), # poids metal suspentes

_F(GROUP_MA='GM1005', FZ= -(7.00/9.60)*4.19*0.887*ksur/102 ,), # poids 1.60 * A(l)

_F(GROUP_MA='GM1011', FZ= -4.19*(0.150*kelu+0.361*ksur)/102 ,), # passerelle chargée a(l)

),);

la charge critique dépend de l'ordre d'écriture des lignes en _F après FORCE_POUTRE=(

ce qui est suspect. Ma solution est pour le moment de tout convertir en FORCE_NODALE.

nota : les modes de flambement sont recherchés après calcul de la matrice de raideur par :

lamda_min= 0.0 ;

lamda_max= 50.0 ;

Mod_flam=MODE_ITER_SIMULT(MATR_A=Mt_raide,

MATR_B=MARG,

NMAX_ITER_SOREN=5000,

TYPE_RESU='MODE_FLAMB',

CALC_FREQ=_F(OPTION='BANDE',

CHAR_CRIT=(lamda_min,lamda_max,),),

VERI_MODE=_F(STOP_ERREUR='NON',),);

Cordialement

jeanpierreaubry

humm

avant le MODE_ITER_SIMULT

vous avez sans doute fait un

MECA_STATIQUE(MODELE=model,CHAM_MATER=material,CARA_ELEM=elemcar,

EXCIT=(_F(CHARGE=ground,),

_F(CHARGE=Ch_ELU_R,),),

OPTION ='SIEF_ELGA',);

si ce MECA_STATIQUE est exécuté seul avec production d'un résultat, en déplacement par exemple, celui ci est il sensible à l'odre des forces réparties ??

juste une question a coté du sujet vous visualisez les résultats avec quoi ?

apalazzi

J_Berthellemy wrote:

Ch_ELU_R =AFFE_CHAR_MECA(MODELE=Structur,
                     FORCE_NODALE=(_F(NOEUD=('N33','N97','N161','N225','N289','N291','N227','N163', 'N99','N35',
                                             'N34','N98','N162','N226','N290','N292','N228','N164','N100','N36',
                                             ),
                                     FZ= -3.67*kelu/(2*102) ,),                   # poids metal des p_de_pont en MN = 3,67 tonnes /2
                                   _F(NOEUD=('N13','N14','N15','N16',),
                                     FZ= -kelu*(2*3.5 + 6.0)/(2*102)  ,),),       # poids des noeuds d'about  et p_de_pont_about
                     FORCE_POUTRE=(
                                   _F(GROUP_MA='GM1005', FZ= -(8.54/9.60)*4.19*0.25*2.6*kelu/102  ,),       # poids de la dalle
                                   _F(GROUP_MA='GM1001', FZ= -1.50*1.20*kelu/102 ,),                              # poids superstructures  
                                   _F(GROUP_MA='GM1001', FZ= -A_Tira*7.85*kelu/102 ,),                          # poids metal tirants
                                   _F(GROUP_MA='GM1003', FZ= -A_Arcs*7.85*kelu/102  ,),                       # poids metal arcs
                                   _F(GROUP_MA='GM1004', FZ= -A_Susp*7.85*kelu/102  ,),                      # poids metal suspentes
                                   _F(GROUP_MA='GM1005', FZ= -(7.00/9.60)*4.19*0.887*ksur/102 ,),         # poids 1.60 * A(l)
                                   _F(GROUP_MA='GM1011', FZ= -4.19*(0.150*kelu+0.361*ksur)/102 ,),      # passerelle chargée a(l)
                            ),);

Hi,

there seems to be a limitation (or a bug) in the application of several loads in the same AFFE_CHAR_MECA: see also http://www.code-aster.org/forum2/viewtopic.php?id=14568, post #15.

I don't know what is the behaviour in these cases, haven't done indeep testing; maybe someone from the developers team can give an exact explanation of the behaviour of CA ?

Bye

J_Berthellemy

jeanpierreaubry wrote:
juste une question a coté du sujet vous visualisez les résultats avec quoi ?

Je visualise la forme des modes avec GMSH et les coefficients d'amplification critique sont dans un fichiers RESU

D'ordinaire je n'utilise pas Aster pour les calculs statiques sur des barres.

je n'ai donc encore jamais testé l'ordre des _F sur des barres en statique.

Je regarderai dès que possible : est-ce faux aussi ?

Cordialement.

J_Berthellemy

apalazzi wrote:
there seems to be a limitation (or a bug) in the application of several loads in the same AFFE_CHAR_MECA

Merci pour cette confirmation

regards.

jeanpierreaubry

NO!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

apalazzi wrote:
there seems to be a limitation (or a bug) in the application of several loads in the same AFFE_CHAR_MECA

THIS IS NOT TRUE

in a single AFFE_CHAR_MECA you can have several FORCE_POUTRE

it works in MECA_STATIQUE

http://www.code-aster.org/forum2/viewtopic.php?id=14568, post #9 by Thomas de Soza

i have never checked if changing the order changes the results

apalazzi

jeanpierreaubry wrote:
NO!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!

[quote=apalazzi]there seems to be a limitation (or a bug) in the application of several loads in the same AFFE_CHAR_MECA

THIS IS NOT TRUE

in a single AFFE_CHAR_MECA you can have several FORCE_POUTRE

it works in MECA_STATIQUE

i have never checked if changing the order changes the results[/quote]

Hi,

please take a look at http://www.code-aster.org/forum2/viewtopic.php?id=14568 , message #15; there's an attachment with a simple test case: please run it and check if the results are correct or not. Note that CA does not complain at all, no errors and no alarms are raised.

I think that the results are not right; however maybe I'm misinterpreting the results, or maybe I've done something wrong in the command file, or some other error unnoticed to me, or maybe this behaviour is explained in the documentation and I've not seen it.

What I see is that the sum of all forces (loads and reactions) is not equal to zero, if you find instead that the CA handles correctly this situation, please let me know.

Bye

Andrea

jeanpierreaubry

i have answered that in the same post!

apalazzi

jeanpierreaubry wrote:
i have answered that in the same post!

Hi,

in that thread the question was about obtaining stresses in beams, and one of the proposed solutions were to define multiple loads in a single AFFE_CHAR_MECA.

However this does not work, in the sense that the results are not correct, as I showed in my test case; and since it's IMHO a legitimate case, it shoud give right results, but it does not.

The problem, there like here, lies in the fact that the loads are not properly applied by AFFE_CHAR_MECA - or at least, AFFE_CHAR_MECA does not behave as I'm expecting it would.

If you instead think that it works and I'm doing something wrong, please show me where's the error in the test case I've posted.

Bye

Andrea

jeanpierreaubry

well

i ran quite a few problems without seeing that tye of error

maybe you could post it again with some comments what is wrong

jean pierre auabry

jeanpierreaubry

if in a given AFFE_CHAR_MECA

you specify a load F1 on a node (element) named A in a first occurence of FORCE_NODALE (FORCE_POUTRE)

then, if in a second occurence you specify a load F2 on the same node (element) A

load F2 will only be applied and F1 ignored

this is what Aster call "SURCHAGE"

and a line like this will be issued in the .mess file

" affectation déjà effectuée du ddl FZ du noeud N241 : on applique la règle de surcharge"

that is probably you think your results are wrong

by the way in your prova_poutre.zip

the .mess file does not like what it should be if it had been run from struttura.comm,

group names are different!!

look a bit like a mess

J_Berthellemy

jeanpierreaubry wrote:
la règle de surcharge

C'est un point important où Aster est différent des autres calculateurs

qui cumulent les charges dans ce cas au lieu de conserver la dernière.

( Most beam calculators add the loads instead of using only the last one ).

Je vais reconsidérer mes calculs à la lumière de cette remarque.

Merci et à bientôt.

apalazzi

jeanpierreaubry wrote:
if in a given AFFE_CHAR_MECA

you specify a load F1 on a node (element) named A in a first occurence of FORCE_NODALE (FORCE_POUTRE)

then, if in a second occurence you specify a load F2 on the same node (element) A

load F2 will only be applied and F1 ignored

So, you agree with me that you can specify more than a single FORCE_NODALE/_F in an AFFE_CHAR_MECA, but only the last one is applied, making this "feature" pretty useless - not to say dangerous. In practice, if you want to apply more than a load (applied with the same keyword) you must specify them in different AFFE_CHAR_MECA.

this is what Aster call "SURCHAGE"

and a line like this will be issued in the .mess file

" affectation déjà effectuée du ddl FZ du noeud N241 : on applique la règle de surcharge"

that is probably you think your results are wrong

In my test case (with FORCE_POUTRE) no warning is raised, and no message is written about that.

by the way in your prova_poutre.zip

the .mess file does not like what it should be if it had been run from struttura.comm,

group names are different!!

look a bit like a mess

In this thread: http://www.code-aster.org/forum2/viewtopic.php?id=15311 I've attached the same test case with the same data but with results up to date.

Bye

Andrea

jeanpierreaubry

apalazzi wrote:
So, you agree with me that you can specify more than a single FORCE_NODALE/_F in an AFFE_CHAR_MECA, but only the last one is applied, making this "feature" pretty useless - not to say dangerous. In practice, if you want to apply more than a load (applied with the same keyword) you must specify them in different AFFE_CHAR_MECA.

of course i do not agree as this NOT TRUE!!!!!!

this only occurs every time you try to impose a new force on every single node (or element) that contains already a load of the same type

this is extremely useful an is not a bad behavior!!!!!

with more experience you will discover why

apalazzi wrote:
this is what Aster call "SURCHAGE"

and a line like this will be issued in the .mess file

" affectation déjà effectuée du ddl FZ du noeud N241 : on applique la règle de surcharge"

that is probably you think your results are wrong

In my test case (with FORCE_POUTRE) no warning is raised, and no message is written about that.

maybe some INFO not properly set in the .comm file

apalazzi

jeanpierreaubry wrote:
of course i do not agree as this NOT TRUE!!!!!!

this only occurs every time you try to impose a new force on every single node (or element) that contains already a load of the same type

this is extremely useful an is not a bad behavior!!!!!

with more experience you will discover why

It's clear that we don't have the same point of view, and at this point there's nothing more to say.

I would have liked an example where such a situation could have been "extremely useful", but probably we wouldn't agree even on that, so let's stop this conversation here.

Bye

Andrea

J_Berthellemy

Bonjour,

La règle de non superposition et de substitution n'est pas un problème dans Aster.

Mais il faut s'en souvenir quand on utile aussi d'autres logiciels !

au lieu de

FORCE_POUTRE=(

_F(GROUP_MA='GM1001', FZ= -1.50*1.20*kelu/102 ,), # poids superstructures

_F(GROUP_MA='GM1001', FZ= -A_Tira*7.85*kelu/102 ,), # poids charpente

il faut écrire

FORCE_POUTRE=(

_F(GROUP_MA='GM1001', FZ= -1.50*1.20*kelu/102 # poids superstructures

-A_Tira*7.85*kelu/102 ,), # poids charpente

et tout rentre dans l'ordre.

Merci encore à J.P. Aubry.

Cordialement.